Creating User Defined Tools in Alphacam

A User-Defined tool is handled differently in Alphacam than other tool types. This option allows you to select a previously drawn geometry profile that will then be used to determine the shape of the tool.

When designing your profile, we recommend that you do the following:

1. When drawing your profile, only draw one half of the profile, then use the Edit | Move, Copy etc. | Mirror command to ensure that the tool profile is symmetrical.

2. Draw a circle (of any diameter) and place it at any place along the tool outline. The center of the circle will determine where the measurement of the tool will begin so that tool length compensation can be properly performed as well as setting the Z level of the tool used in NC Code programming.





3. Draw a straight horizontal line (of any length) so that it intersects the tool outline. This will specify the diameter of the tool that should be used with G41/42 offset compensation.

4. Go to the Machine drop down menu, select Define Tool. 

5. Next, select User Defined.

Once you select the profile that is to be used to define this tool, you may see the following warning: 

This dialog is only informing you that Alphacam has detected a Line and Circle that are attached to the profile to determine the reference diameter and the Z Level of the tool. You will not see this warning if both a Line and Circle do not exist along the profile.

Next you will see the following dialog:

This dialog has the following options:

Tool Number - this number will be the number that is displayed in the NC Code to represent this tool.

Offset Number - this number will be the offset number that is used in the NC Code for this tool.

Length - this displays the length of the tool. This value will reflect the distance from the center of the circle to the top of the profile if a circle was added to the profile.

Diameter - this displays the diameter of the tool. This value will reflect the width of the profile at the intersection of the horizontal line through the profile if a line was added to the profile.

Special - this is not valid for a User-Defined type.

Units - this allows you to specify that the measurements of this tool are of either the Inch (") type or the Metric (mm) type.

Spindle Rotation - this allows you to specify whether this tool rotates in a Clockwise (CW) or Counterclockwise (CCW) direction. Cut Depths - this allows you to specify the typical pecking depth each cut should make with this tool as well as the maximum depth that this tool can go.

Feeds and Speeds - this allows you to specify that this tool uses either calculate feed movements, or a fixed speed and feed. If you select to use a calculated speed, you must enter the feed speed revolution of the tool. If you select to use a fixed speed, you must enter the typical desired Spindle Speed, Fixed Feed rate and the Fixed Down Feed rate.

Tool Notes - This allows you to specify notes that should appear in the NC Code that is generated when this tool is used. 

• Tool Holder - this allows you to specify the length and diameter of the tool holder for this tool. Clicking on the default... button allows you to specify the default tool holder values that will be displayed here.

• Tool Tip to Guide Line Length - this allows you to specify the distance, from the tip of the tool to the top of the tool holder. This value is calculated by Alphacam, but can be modified by the user.

• Tool Holder Graphics - this allows you to specify that this tool should display the tool holder graphics when shown in either the Simulation or the Solid Simulation.

<<< Back to Alphacam Tips & Tricks


Dystrybutor

Zapraszamy na naszą stronę:

www.dps-software.pl

 

Vero jest wiodącym dostawcą oprogramowania do meblarstwa, branży metalowej i obróbki kamienia.